What am I doing wrong? Modal Frequency Responce

[viktor_velichko]

Hello dear colleagues. I tryed to do harmonic analysis by applying base motion displacement. But I got strange result - I did't get responce

What am I doing wrong? I attach the file.

I maked another study with slight changes and got a response. But I do not understand that I have substantially changed.

[John_Holtz]

Hi @viktor_velichko 

The first image (where only the end is deforming) is from Analysis 7 in your model. The second image with the correct result is from Analysis 3 - Copy.

The enforced displacement in Analysis 7 is assigned to a Load Factor Table 6. This table is causing a problem for unknown reasons. If you replace the Load Factor table with a New Table (as was used in Analysis 3 - Copy) instead of using Table 6, then you get the same result as in Analysis 3 - Copy.

[viktor_velichko]

Yes, you're right. I'm sorry that I didn't write in more detail. I have been suffering with this problem for a long time. How can I undestand what way is right, what wrong. It's just simple exsample. When I tryed this doing with huge problem I repeaded all like Analysis 3 - Copy and got wrong. The picture was like Analysis 7 Are there any rules for using enforced displacement and accelerations for Modal Frequency Responce analysis? How does this Tables right use ?

[John_Holtz · Accepted solution]

I think your input is okay, or at least should be acceptable, and therefore it should work. Since it does not work, the question becomes "what input is unexpected and therefore not programmed to be handle"? For example,

• Is the problem that the load table has multipliers of 0 for a portion of the curve? (Why would someone apply a load and then say it is zero? I bet a programmer would not think of that as a real-life possibility and did not program something correctly to handle it.) I suggest not using a value of 0 for a segment of the load history. (Using 0 for one end point of a segment should be okay. I think having two zeros in two rows may be a problem.)
• Is the problem that the dynamic setup goes from frequencies of 0 to 1000? (Why would someone vibrate the model at a frequency of zero? I bet a programmer would not think of that as a real-life possibility and did not program something correctly to handle it.) I would set a lower frequency at some value larger than 0.

Let us know what happens.

[viktor_velichko]

John, you have a lot of experience with programmers 🙂

Yes, the first assumption turned out to be true. The second assumption is not. All the same, they thought about it.

When I changed 0 to a close value, the response appeared. Thank you very much!

But this is a bug and I would like to convey it to the developers. Could you tell me how to do this?

My vibration load is set in one frequency range through displacements, in another through accelerations. Like this:

1 - 10 Hz - 1 mm

10 - 100 Hz - 9.8 m/s^2

Now I suspect that requesting them through two different loads will fail (I tried to do this, but I got false results). What is the best way for me to do this? Translate displacements into accelerations or split into two analyzes with different loads? The next step I would like to calculate vibration fatigue, but I do not yet have experience on this module of Inventor Nastran.

[John_Holtz]

Here's an update. Someone on the development team looked at the model. They discovered another solution. Instead of this input table (for the load) that did not give correct results:

0	0
1	0
5	1
900	1
1000	1

this input table gives correct results:

0	0
0.99	0
5	1
900	1
1000	1

Very strange! The issue has been logged with the developers.

[viktor_velichko]

Ok! Thank you!

[pclementsADJA4]

Has there been any update around this issue? I am running Nastran 2022 Version 16.0.087 and still seing this issue.

The load table is per below, how should I modify this? Maybe a T=0.1, LSF = 0.99?